HEIDENHAIN TNC 410 - Manual (Page 104)

91 HEIDENHAIN TNC 410
6.5 P
ath Cont
ours — P
olar Coor
dinat
es Example: Helix
Define the blank form
Define the tool
Call the tool
Retract the touch probe
Pre-position the tool
Transfer the last programmed position as the pole
Move to working depth
Approach the contour on a circular arc with tangential
connection
Helical interpolation
Depart the contour on a circular arc with tangential connection
Retract in the tool axis, end of program
Identify beginning of program section repeat
Enter the thread pitch as an incremental IZ dimension
Program the number of repeats (thread revolutions)
0 BEGIN PGM HELIX MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+5
4 TOOL CALL 1 Z S1400
5 L Z+250 R0 FMAX
6 L X+50 Y+50 R0 F MAX
7 CC
8 L Z-12.75 R0 F1000 M3
9 APPR CT X+18 Y+50 CCA180 R+2
RL F100
10 CP IPA+3240 IZ+13.5 DR+ F200
11 DEP CT CCA180 R+2 R0
12 L Z+250 R0 FMAX M2
13 END PGM HELIX MM
To cut a thread with more than 16 revolutions
...
8 L Z-12.75 R0 F1000
9 APPR CT X+18 Y+50 CCA180 R+2 RL F100
10 LBL 1
11 CP IPA+360 IZ+1.5 DR+ F200
12 CALL LBL 1 REP 24
13 DEP CT CCA180 R+2 R0
X
Y
50
50
CC
100
100
M64 x 1,5